CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

icoFOAM don't calculate right

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   December 10, 2012, 03:03
Question icoFOAM don't calculate right
  #1
New Member
 
Wang Han
Join Date: May 2012
Location: Shanghai China
Posts: 21
Rep Power: 4
whyingwang is on a distinguished road
Hello FOAM users,
Recently I use icoFOAM to claculate a channel flow,like the picture show,
I use ICEM to make a struct-mesh,see below.

Later,I use icoFOAM,one of the two pipes is inlet another is outlet.
But I failed.After 2000 steps,It shows that the velocity still stay at inlet,like the picture shows.The red only can be see at one pipe.

Please,Who can tell me why?
Thanks.
whyingwang is offline   Reply With Quote

Old   December 10, 2012, 03:38
Default
  #2
Member
 
Robert
Join Date: Aug 2012
Location: Berlin
Posts: 74
Rep Power: 4
vainilreb is on a distinguished road
My first quick guess would be:

You set the channel walls to "wall" - which usually means the velocity at the boundary is "uniform (0 0 0)". Have you had a look at a cross-section through the channel? There might be high flow velocities in the middle of the channel. This is what you see at the inlet cross-section, too.
vainilreb is offline   Reply With Quote

Old   December 10, 2012, 04:06
Default
  #3
New Member
 
Wang Han
Join Date: May 2012
Location: Shanghai China
Posts: 21
Rep Power: 4
whyingwang is on a distinguished road
Quote:
Originally Posted by vainilreb View Post
My first quick guess would be:

You set the channel walls to "wall" - which usually means the velocity at the boundary is "uniform (0 0 0)". Have you had a look at a cross-section through the channel? There might be high flow velocities in the middle of the channel. This is what you see at the inlet cross-section, too.
Thanks For your answer.But, actually It's velocity at the middle of the channel is nearly zero,see below . My inlet velocity is 1.9m/s.
whyingwang is offline   Reply With Quote

Old   December 10, 2012, 04:33
Default
  #4
Member
 
Robert
Join Date: Aug 2012
Location: Berlin
Posts: 74
Rep Power: 4
vainilreb is on a distinguished road
Well, at least there IS a flow profile. Please post your BC files, especially p and U!
vainilreb is offline   Reply With Quote

Old   December 10, 2012, 08:34
Default
  #5
New Member
 
Wang Han
Join Date: May 2012
Location: Shanghai China
Posts: 21
Rep Power: 4
whyingwang is on a distinguished road
Quote:
Originally Posted by vainilreb View Post
Well, at least there IS a flow profile. Please post your BC files, especially p and U!
OK,Here is my 0 time files
----------------------------------------------------------------------------------------------------------------------------
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 2 -2 0 0 0 0];

internalField uniform 0;

boundaryField
{
inletWall
{
type zeroGradient;
}
outletWall
{
type fixedValue;
value uniform 101.630;
}
upWalls
{
type zeroGradient;
}
inPipe
{
type zeroGradient;
}
outPipe
{
type zeroGradient;
}
downWalls
{
type zeroGradient;
}
outerWalls
{
type zeroGradient;
}
}
---------------------------------------------------------------------------------------------------------------------------
FoamFile
{
version 2.0;
format ascii;
class volVectorField;
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 1 -1 0 0 0 0];

internalField uniform (0 0 0);

boundaryField
{
inletWall
{
type fixedValue;
value uniform (0 0 -1.9099);
}
outletWall
{
type zeroGradient;
}
upWalls
{
type fixedValue;
value uniform (0 0 0);
}
inPipe
{
type fixedValue;
value uniform (0 0 0);
}
outPipe
{
type fixedValue;
value uniform (0 0 0);
}
downWalls
{
type fixedValue;
value uniform (0 0 0);
}
outerWalls
{
type fixedValue;
value uniform (0 0 0);
}
}

// ************************************************** *********************** //
whyingwang is offline   Reply With Quote

Old   December 10, 2012, 08:54
Default
  #6
Member
 
Robert
Join Date: Aug 2012
Location: Berlin
Posts: 74
Rep Power: 4
vainilreb is on a distinguished road
Okay, first thing I see is your inlet velocity.
(0 0 -1.9099) points in negative Z-direction which is, according to the coordinate system, orthogonal to your inlet patch - because Y is the vertical axis!
Try (0 -1.9099 0).

And why is your pressure at the outlet so much higher than in the internal field? Uniform 0 for internal field means you've got ambient pressure level in the internal. Uniform 101.630 at the outlet means you've got 101.63 N/mē overpressure at the outlet. This probably won't work if you want the fluid to leave your channel at this patch. I suggest you try uniform 0 there, too.

Hope this will fix your problem.
vainilreb is offline   Reply With Quote

Old   December 10, 2012, 09:42
Default
  #7
New Member
 
Wang Han
Join Date: May 2012
Location: Shanghai China
Posts: 21
Rep Power: 4
whyingwang is on a distinguished road
Quote:
Originally Posted by vainilreb View Post
Okay, first thing I see is your inlet velocity.
(0 0 -1.9099) points in negative Z-direction which is, according to the coordinate system, orthogonal to your inlet patch - because Y is the vertical axis!
Try (0 -1.9099 0).

And why is your pressure at the outlet so much higher than in the internal field? Uniform 0 for internal field means you've got ambient pressure level in the internal. Uniform 101.630 at the outlet means you've got 101.63 N/mē overpressure at the outlet. This probably won't work if you want the fluid to leave your channel at this patch. I suggest you try uniform 0 there, too.

Hope this will fix your problem.
yes,Thank you Very Much,vainilreb.
I get the reason now.
whyingwang is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Density in icoFoam Densidad en icoFoam manuel OpenFOAM Running, Solving & CFD 8 September 22, 2010 04:10
calculate values for eps and k from Re or u????? sbar OpenFOAM Pre-Processing 5 August 16, 2010 04:10
Kubuntu uses dash breaks All scripts in tutorials platopus OpenFOAM Bugs 8 April 15, 2008 07:52
IcoFoam parallel woes msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 02:58
How to calculate Torque for francis turbine manish CFX 4 March 15, 2007 03:57


All times are GMT -4. The time now is 04:32.